Roughing toolpath Z ramp?

[jdwykrent]

I am carving a file out of aluminum. My depth of cut is .002. I would like to ramp the Z plunge but can't figure out how... I know how in a profile cut but can't seem to figure it out in a roughing or finishing cut.

I'm using Aspire 4.5

[MogulTx]

Jeff,

I can't figure that one out either- and would like to know the solution for the same type application.... cutting aluminum... I will monitor this thread, but if you find something out, let me know, please...

( I/we ought to write Brady Watson an email. He is VERY versatile and works in aluminum - and offers advice on many topics.... he may just be a fantastic resource on this... I will send him a PM and see what he says. I will post the response info back here if her can help.)

Monty

[Brady Watson]

Brady

Do you know a way to set up a ramping scenario for a 3D roughing and finishing path in Aspire? For doing aluminum, it would be a very useful attribute. I don't do a LOT of 3D work in aluminum, but I am working on roughing then finishing a piece and I was seeing Jeff Wykrent also posting looking for a way to do that... I have not sent an email to Vectric just yet....

Thanks for any insight you might have.

Best Regards,


The best thing I could advise is to 'sneak up on it' - meaning...First do the profile pass and clear away the perimeter portion. Then do your 3D roughing using a smaller stepover value than you would normally use. I'd say pull it down to like 15% instead of 40%. Keep step down depths low - as in .01-.04" per pass - but use your own discretion here, erring on the side of being conservative. Reduce your roughing allowance from the default .04 to .015 or .02". If it isn't possible to remove the perimeter waste material because you want to use tabs, then you'll want to make 2 profile passes; one @ 0 and another at let's say .03" allowance (larger) to create a valley that is free & clear of material for the finishing tool - such that it will NEVER contact the scrap material when machining. Don't use a smaller tool for the profile than your 3D finish - think about this...and siamese your tabs on these two profile passes...

Care must be taken to make sure that the ball end tool isn't going to nosedive into cavernous features that the roughing tool missed AND the boundary vector MUST be checked with simulation to make sure your tool isn't going to 'fall off the side' when finish machining. This isn't a big deal if your ball end mill is long enough AND you cleared away the perimeter waste as directed. It is often necessary to do a 'rough 3D finish' using a ball smaller than the square end mill used for roughing @ 25% stepover that can take plunging down into any cavernous features without breaking. Then follow up with your final finish ball tool @ smaller diameter and 10% or lower stepover. You may find the Aspire tutorial regarding 'Rest Machining' helpful for identifying any features that may be too much for a given tool, prompting you to split up your 3D finishing passes as 2 operations.

The trick here is going to be hold down. If you can drill/tap and bolt it from the back using a 'carrier board', that is best, but part specific. DS/carpet tape will most likely fail from the AL getting heat soaked and this can be dangerous for you and/or catastrophic for your part. Hold down MUST be rock solid. You can white glue paper to the AL and another substrate to get it locked down - then pry apart after. Get creative. You can always use Kreg screws and tabs...no drywall screws, right kids?

SAFETY GLASSES NOT OPTIONAL!!! Even with the machine OFF chips, when disturbed, will reverse static polarity and SHOOT YOU STRAIGHT IN THE EYES!!! (I know this from experience)

Keep a cool tool - O-flute for roughing if you can, HSS 2-flute end mill is OK too. Try not to overheat the tool. Compressed air blowing on bit @ 20 psi works well. Football inflator & some brass fittings work well. 50/50 denatured & water occasionally spritzed on the part helps with good airflow (evaporation is a cooling process...).

One more thing...VR settings. Adjust your slow corner speed down to 30% to reduce shock loads @ direction changes. This will cushion movement a bit, which is helpful when using carbide (aka crystalline) tools. HSS is sharper than carbide but doesn't last as long...but they bend before they break and absorb harmonics that comes with cutting metal...carbide does not.

Cutting AL many times 'sounds all wrong' if you primarily cut wood & plastic. Just let the tool do the work & don't be afraid to adjust the tool to get it cutting as smoothly as possible. Sometimes it makes sense to do a dry run in something like wood, just to check yourself before you get into that billet...

-B